Extruded Boss/Base and Extruded Cut¶
Extrudes the closed profiles of a sketch to add material (Extruded Boss/Base) or remove it (Extruded Cut).
Features tab > Extruded Boss/Base or Extruded Cut, or right-click a sketch > Extruded Boss/Base or Extruded Cut.

Creating an Extrude¶
- Select the sketch in the design tree or the graphics area. If no sketch is selected, the last sketch, when no feature uses it yet, is taken.
- Click Extruded Boss/Base or Extruded Cut.
- Set the end condition and the Depth in Direction 1.
- Click OK or press Enter.
If there is no sketch to use, the command starts a sketch first. Sketch the profile, then click Exit Sketch to continue. Clicking the command while editing a sketch exits the sketch and continues.
The view turns to Isometric when the page opens, or to another isometric corner if the model hides the sketch. See Exiting a Sketch.
A new boss starts as Blind, 10 mm deep (0.5 in in inch parts). A new cut starts as Through All with Reverse direction on.
Output¶
- Operation
- Join adds the extrude to the bodies it touches. Cut removes it from every body it passes through. Intersect keeps only what each body it overlaps has in common with it. New body makes it a separate body. A feature that still has its automatic name is renamed to match, for example Boss-Extrude1 to Cut-Extrude1. An Intersect feature cannot be patterned or mirrored.
Sketch¶
- Sketch
- The profile sketch. Select it in the design tree or the graphics area.
- Regions
- What is extruded: closed areas of the sketch, and planar faces of the model. It starts with every area the sketch's closed profiles cover, shaded. Select inside an area, or a planar face, in the graphics area to add it, and again to remove it. Areas side by side are joined. Curves that cross split each other into areas, with no shared point needed, so a line drawn across a rectangle or a circle makes two areas. Each face is extruded from its own plane, along its normal, and needs no sketch. A face on the sketch's plane stops at the sketch's curves on it: the sketch's areas are extruded only when they are selected too, and of a face split by a line, only the side where it was selected. A region keeps its place when the sketch changes; one no longer in the sketch shows in red, with a warning. To extrude an area bounded partly by model edges, add the edges to the sketch with Convert Entities, then select the area.
From¶
The section is folded while the extrude starts at the sketch plane. Click its header to open it.
- Start
- Where the extrude starts. Sketch Plane: the sketch's plane. Offset: a plane parallel to it, the Offset away along direction 1 (negative: the other way). Vertex: level with a vertex or sketch point. Surface/Face/Plane: a plane or planar face, which may be at an angle to the sketch; the profile is carried onto it along the extrude. Depths are measured from the start. From a surface, a Blind extrude ends at the start plane carried the depth on, and there is no draft, Mid Plane or Through All - Both.
Direction 1¶
The list at the top of the section sets the end condition, how far the extrude goes. The arrow button beside it is Reverse direction.
| Option | Extent |
|---|---|
| Blind | To the Depth |
| Through All | Through the whole part, in one direction |
| Through All - Both | Through the whole part, both ways from the sketch plane |
| Mid Plane | Half the Depth each side of the sketch plane |
| Up To Next | Up to the next material it meets; a cut, through the first material it meets |
| Up To Vertex | Level with the vertex or sketch point in Vertex |
| Up To Surface | Up to the face or plane in Up to |
| Offset From Surface | Up to the face or plane in Up to, stopped the Offset short of it (or past it) |
| Up To Body | Up to the body in Up to |

- Reverse direction
- The arrow button beside the end condition. Extrudes to the other side of the sketch plane. Not shown with Mid Plane, Through All - Both or Up To Vertex.
- Up to
- For Up To Surface and Offset From Surface, a plane or faces to end at. One face of a plane, cylinder, cone, sphere or torus is extended to cover the profile. Several faces, or a face of another kind (a spline surface or a variable blend), are used as they are: the profile must land on them, and no other face may be in the way. For Up To Body, any face of the body; the extrude ends where it enters that body. Not used by the other end conditions.
- Tangent faces
- Up To Surface and Offset From Surface only. Also ends at the faces tangent to the selected ones, such as the fillets that run off a top face.
- Offset
- Offset From Surface only. Stops this far short of the surface; with the arrow button beside it (Reverse offset), this far past it. The end is a surface parallel to the one selected: for one plane, or one face of a plane, cylinder, cone, sphere or torus.
- Translate surface
- Offset From Surface only. Moves the surface along the extrude by the offset instead, keeping its shape: the end follows the faces at a fixed height. Works with any faces, several or tangent ones and spline faces included.
- Depth
- The depth, in the part's units. Used by Blind and Mid Plane. Accepts an equation or a variable name.
- Along a direction
- Extrudes along the linear edge, face, plane or axis in Direction instead of square to the sketch; the X, Y and Z buttons pick an axis. The caps stay parallel to the sketch, and depths are measured along the direction. It must not lie in, or nearly in, the sketch's plane. No draft along a direction.
- Draft angle
-
Tapers the side walls from the sketch plane, narrowing away from it, in degrees. Leave empty, or
0, for no draft. The angle must be below 89°. When the extrude goes both ways (Mid Plane, Through All - Both or a Direction 2 depth), each side narrows away from the sketch plane. With Through All, the drafted extrude ends just past the far side of the part. With the Up To end conditions, it is drafted as far as it goes, then cut back the same way.
- Draft outward
- The button beside Draft angle. The side walls widen away from the sketch plane instead.
Direction 2¶
Turned on by the check box in its header. The extrude the other way from the start: Blind by its Depth, Through All, Up To Next, Up To Vertex, Up To Surface, Offset From Surface or Up To Body, with the same fields as Direction 1. Not used with Mid Plane or Through All - Both.
An Extruded Cut removes material from every body it passes through. If it misses them all, the feature shows the warning "The cut does not intersect the model."
When an Extrude Fails¶
If the extrude cannot be built, the page shows the reason. Common causes:
- The sketch has no closed profile.
- With Up To Surface or Up To Body, the extrude does not reach the surface or body, or part of the profile misses it and would run on past it. Turn on Reverse direction if it lies the other way.
- With a Draft angle, the drafted side walls meet before the end of the extrude. Use a smaller angle or depth, or turn on Draft outward.